Show last authors
1 {{box cssClass="floatinginfobox" title="**Contents**"}}
2 {{toc/}}
3 {{/box}}
4
5 Depending on the current FEM-Design module you can do different calculations: displacement, internal forces, stresses, stability, imperfections, stability analysis, eigenfrequencies and/or seismic analysis. Some extra settings such as cracked-section analysis, non-linear behaviour etc. are also available for certain modules.
6
7 (% class="table-hover" style="width:610px" %)
8 |(% style="width:259px" %)Analysis type/settings|(% style="text-align:center; width:77px" %)[[image:1585304282722-904.png]]|(% style="text-align:center; width:62px" %)[[image:1585304287939-388.png]]|(% style="text-align:center; width:69px" %)[[image:1585304293078-535.png]]|(% style="text-align:center; width:70px" %)[[image:1585304298027-412.png]]|(% style="text-align:center; width:70px" %)[[image:1585304303530-165.png]]
9 |(% style="width:259px" %)Analysis for load cases|(% style="text-align:center; width:77px" %)[[image:1585304316868-130.png]]|(% style="text-align:center; width:62px" %)[[image:1585304325317-999.png]]|(% style="text-align:center; width:69px" %)[[image:1585304325976-532.png]]|(% style="text-align:center; width:70px" %)[[image:1585304326683-198.png]]|(% style="text-align:center; width:70px" %)[[image:1585304335642-255.png]]
10 |(% style="width:259px" %)Analysis for load combinations|(% style="text-align:center; width:77px" %)[[image:1585304320572-882.png]]|(% style="text-align:center; width:62px" %)[[image:1585304324426-152.png]]|(% style="text-align:center; width:69px" %)[[image:1585304345360-694.png]]|(% style="text-align:center; width:70px" %)[[image:1585304337095-717.png]]|(% style="text-align:center; width:70px" %)[[image:1585304348201-717.png]]
11 |(% style="width:259px" %)Analysis for maximum of  load groups|(% style="text-align:center; width:77px" %)[[image:1585304322886-289.png]]|(% style="text-align:center; width:62px" %)[[image:1585304338474-309.png]]|(% style="text-align:center; width:69px" %)[[image:1585304346672-963.png]]|(% style="text-align:center; width:70px" %)[[image:1585304343412-989.png]]|(% style="text-align:center; width:70px" %)[[image:1585304350465-766.png]]
12 |(% style="width:259px" %)Imperfections|(% style="text-align:center; width:77px" %) |(% style="text-align:center; width:62px" %) |(% style="text-align:center; width:69px" %) |(% style="text-align:center; width:70px" %)[[image:1585304355098-291.png]]|(% style="text-align:center; width:70px" %)[[image:1585304356971-553.png]]
13 |(% style="width:259px" %)Second order analysis|(% style="text-align:center; width:77px" %) |(% style="text-align:center; width:62px" %) |(% style="text-align:center; width:69px" %) |(% style="text-align:center; width:70px" %)[[image:1585304366475-455.png]]|(% style="text-align:center; width:70px" %)[[image:1585304368061-608.png]]
14 |(% style="width:259px" %)Stability analysis|(% style="text-align:center; width:77px" %) |(% style="text-align:center; width:62px" %) |(% style="text-align:center; width:69px" %) |(% style="text-align:center; width:70px" %)[[image:1585304451552-428.png]]|(% style="text-align:center; width:70px" %)[[image:1585304456840-851.png]]
15 |(% style="width:259px" %)Eigenfrequencies|(% style="text-align:center; width:77px" %)[[image:1585304446676-611.png]]|(% style="text-align:center; width:62px" %)[[image:1585304448716-182.png]]|(% style="text-align:center; width:69px" %)[[image:1585304455595-358.png]]|(% style="text-align:center; width:70px" %)[[image:1585304450524-253.png]]|(% style="text-align:center; width:70px" %)[[image:1585304452997-875.png]]
16 |(% style="width:259px" %)Seismic analysis|(% style="text-align:center; width:77px" %) |(% style="text-align:center; width:62px" %) |(% style="text-align:center; width:69px" %) |(% style="text-align:center; width:70px" %)[[image:1585304442660-117.png]]|(% style="text-align:center; width:70px" %)[[image:1585304445044-144.png]]
17 |(% style="width:259px" %)Non-linear behavior|(% style="text-align:center; width:77px" %)[[image:1585304434090-131.png]]|(% style="text-align:center; width:62px" %)[[image:1585304436010-650.png]]|(% style="text-align:center; width:69px" %)[[image:1585304425716-631.png]]|(% style="text-align:center; width:70px" %)[[image:1585304429309-891.png]]|(% style="text-align:center; width:70px" %)[[image:1585304427706-966.png]]
18 |(% style="width:259px" %)Cracked-section analysis|(% style="text-align:center; width:77px" %)[[image:1585304432576-696.png]]|(% style="text-align:center; width:62px" %)[[image:1585304430965-519.png]]|(% style="text-align:center; width:69px" %)[[image:1585304423428-601.png]]|(% style="text-align:center; width:70px" %)[[image:1585304419438-855.png]]|(% style="text-align:center; width:70px" %)[[image:1585304421638-598.png]]
19 |(% style="width:259px" %)Peak**//-smoothing algorithm//**|(% style="text-align:center; width:77px" %)[[image:1585304384420-951.png]]|(% style="text-align:center; width:62px" %)[[image:1585304385724-492.png]]|(% style="text-align:center; width:69px" %)[[image:1585304386991-527.png]]|(% style="text-align:center; width:70px" %)[[image:1585304388291-423.png]]|(% style="text-align:center; width:70px" %)[[image:1585304390530-213.png]]
20
21 Table: Analysis features by FEM-Design Modules
22
23 Analysis can be done independently from any design calculations by entering to [[image:1585304470015-166.png]] tabmenu and clicking [[image:1585304477784-655.png]] //Calculate// command, or together with designs (RC, Steel or Timber) with the same command.
24
25 [[image:1585304484190-908.png]]
26
27 Figure: Analysis calculations
28
29 Analysis settings contain general and calculation-dependent settings. This chapter summarizes these settings and their effect on the result. Clicking //OK// runs Analysis according to the settings and selected calculation types. Other chapters introduce the display of results and their documentation (such as listing results in tables).
30
31 = {{id name="General Analysis Settings"/}}General Analysis Settings =
32
33 == Finite Element Types ==
34
35 In the 3D modules, you can choose between “standard” and “accurate” 2D element types. With standard elements you can run 4-times faster but less accurate analysis than with the fine elements.
36
37 == Peak Smoothing ==
38
39 To solve singularity problem in analysis results (internal forces), it is not enough to create peak smoothing regions in the finite element mesh. The use of the peak smoothing algorithm in the calculations have to be allowed. Without that permission, peak smoothing regions cause only mesh refinements (densifications) around objects.
40
41 [[image:1585304517715-300.png]]
42
43 Figure: Peak smoothing algorithm for Analysis
44
45 == Setup calculation by load combinations ==
46
47 The calculation of the load combinations can be run with different options. They can be set in Calculations dialog by selecting the Load combination items and clicking [[image:1585304536084-353.png]] on //Setup by load combinations//.
48
49 [[image:1585304541411-585.png]]
50
51 The User has the opportunity to choose
52
53 * Which load combination should be calculated (Calc)
54 * Non-linear elastic calculation (NLE),
55 * Plastic analysis (PL),
56 * Non-linear soil (NLS),
57 * Cracked-section analysis (Cr.),
58 * Second order analysis (2nd),
59 * Imperfection calculation (Im., the selected shape will be taken into account in Second order analysis)
60
61 for each Load combinations.
62
63 |(% style="width:89px" %)[[image:light.png]]|(% style="width:1401px" %)For example, in practice it can be useful to set 2^^nd^^ order analysis only for the ULS and Cracked-section analysis only for the SLS combinations.
64
65 === **Non-Linear Behavior** ===
66
67 Non-linear behavior of supports (e.g. uplift), connections and truss members (e.g. tension-only) can be considered in analysis calculations (for load-combinations, imperfections and stability) by ticking //NL// checkbox at //Calculations > Analysis > Load combinations > Setup load combinations//.
68
69 |(% style="width:89px" %)[[image:light.png]]|(% style="width:1401px" %)“Uplift” can be modeled both in 2D and 3D design modules by defining compression-only //support/connection// (tension = 0 (free)) and by selecting non-linear calculation for a load combination.
70
71 There is a possibility for the user to set the maximum iteration number of nonlinear calculation in //Non-linear calculations //tab in// Setup load combination calculation// dialog.
72
73 [[image:1585304645669-954.png]]
74
75 === **Plastic Analysis                             ** ===
76
77 In FEM-Design 3D Structure there is a plastic calculation option by the setup of load combinations.
78
79 Plastic calculation is available for trusses, supports and connections and edge connections of all shell elements (Plane plate and wall, Profiled plate and wall, Timber plate and wall, Fictitious shell).
80
81 [[image:1585304663813-715.png]]
82
83 The options above are considered only for load combinations calculated as non-linear elastic. //Plastic //behaviour is considered for load combinations calculated as non-linear elastic + plastic. See more details in the next chapter.
84
85 For further information check the [[documentation>>url:http://download.strusoft.com/FEM-Design/inst170x/documents/diaphragm_and_plastic_theory.pdf]].
86
87 === **Cracked-Section Analysis** ===
88
89 Cracked-section analysis means that the displacement of RC plates, walls, columns and beams can be calculated based on their cracked state and designed reinforcement.
90
91 [[image:1585304697014-172.png]]
92
93 Figure: Iteration steps of cracked-section analysis
94
95 Cracked section analysis for load combinations is available by ticking the //Cr. //checkbox at //Analysis > Calculations > Load combinations > Setup load combinations// > //By load combinations//
96
97 The iteration process settings available at //Analysis > Calculations > Load combinations// > //Non-linear calculations//:
98
99 (% style="text-align:center" %)
100 [[image:1585304708665-594.png]]
101
102 * **One load step in % of the total load** (= number of load steps):
103 For example, 20% means 5 load steps (= 100/20[%]). Less percentage generates more steps and more running time.
104 * **Maximum iteration number:**
105 The value must be in range 1 and 100.
106 * **Allowed displacement error [%]:**
107 Iteration ends, when the relative displacement error becomes less than the allowed value.
108
109 === **Second Order Analysis** ===
110
111 In the [[image:1585304738723-114.png]] and [[image:1585304744269-673.png]] modules, 2^^nd^^ order theory can be applied for load combination calculations of 3D structures. The 2^^nd^^ order analysis considers the placement of the loads that changes together with the displacement, so it results additional moments derived from the new load positions.
112
113 To allow the 2^^nd^^ order analysis for load combinations, just tick the //2ND// checkbox at //Calculations > Analysis > Load combinations > Setup load combinations// //>// //By load combinations//
114
115 |(% style="width:89px" %)[[image:light.png]]|(% style="width:1401px" %)(((
116 The 2^^nd^^ order analysis is recommended to be done together with imperfection calculation. In //Setup load combinations// dialog, choose load combinations which you would like to apply the 2^^nd^^ order theory for, and give the number of imperfection shape (simultaneous or previous calculation for imperfection is needed) you would like to consider for the 2^^nd^^ order analysis.
117
118 [[image:1585304779623-853.png]]
119 )))
120
121 |(% style="width:113px" %)[[image:warning.png]]|(% style="width:1377px" %)If the loads are too large when using second order analysis, the program stops the calculations with an error message.
122
123 == Diaphragm calculation ==
124
125 If at least one diaphragm is defined in the structure, the user can choose one of the following diaphragm calculation options:
126
127 * None
128 * Rigid membrane
129 * Fully rigid
130
131 The difference between them is demonstrated by the following pictures. See details in the [[documentation>>url:http://download.strusoft.com/FEM-Design/inst170x/documents/diaphragm_and_plastic_theory.pdf]].
132
133 [[image:1585304848899-842.png]]
134
135 = {{id name="Analysis for Construction stages"/}}Analysis for Construction stages =
136
137 (% class="box infomessage" %)
138 (((
139 For further information see:
140 • [[Structure definition of Construction stages>>doc:Manuals.User Manual.Structure definition.Construction stages (Geometry).WebHome]].
141 • [[Load definitions for Construction stages>>doc:Manuals.User Manual.Loads.WebHome||anchor="Construction stages"]]
142 • [[Analysis for Construction stages>>doc:Manuals.User Manual.Analysis.WebHome||anchor="Analysis for Construction stages"]]
143 )))
144
145
146 User can start the construction stage calculation at Analysis/Calculation/Construction stages. There is two calculation method, so called //Incremental “Tracking” method// and //“Ghost” structure method.//
147
148 When incremental method is chosen, the model is built stage-by-stage. In case of “ghost” structure method the full structure is in the calculation, but stiffness of those structural parts which aren’t in the specific stage is highly reduced.
149
150 [[image:1585817052945-991.png]]
151
152 //Incremental “Tracking” method~://
153
154 [[image:1585817079457-517.png]]
155
156 //“Ghost” structure method~://
157
158 [[image:1585304895405-781.png]]
159
160 = {{id name="Analysis for Load Cases and Combinations"/}}Analysis for Load Cases and Combinations =
161
162 Analysis calculations can be done by load case and/or load combination. The next table summarizes the results available for load cases and load combinations by FEM-Design modules.
163
164 [[image:1585304949928-797.png]]
165
166 Figure: Starting analysis for load cases and/or load combinations
167
168 (% class="table-hover" style="width:832px" %)
169 |(% style="width:258px" %)Analysis result|(% style="text-align:center; width:140px" %)[[image:1585304956671-742.png]]|(% style="text-align:center; width:119px" %)[[image:1585304961773-996.png]]|(% style="text-align:center; width:103px" %)[[image:1585304967386-132.png]]|(% style="text-align:center; width:106px" %)[[image:1585304972170-610.png]]|(% style="text-align:center; width:103px" %)[[image:1585304976957-116.png]]
170 |(% style="width:258px" %)**//Translational displacements//**|(% style="text-align:center; width:140px" %)(((
171 [[image:1585304993442-804.png]]
172
173 (Plate/Beam)
174 )))|(% style="text-align:center; width:119px" %)(((
175 [[image:1585305071358-191.png]]
176
177 (Wall)
178 )))|(% style="text-align:center; width:103px" %)(((
179 [[image:1585305065486-862.png]]
180
181 (Wall)
182 )))|(% style="text-align:center; width:106px" %)[[image:1585305037909-452.png]]|(% style="text-align:center; width:103px" %)[[image:1585305034474-161.png]]
183 |(% style="width:258px" %)**//Rotational displacements//**|(% style="text-align:center; width:140px" %)(((
184 [[image:1585304995179-133.png]]
185
186 (Plate/Beam)
187 )))|(% style="text-align:center; width:119px" %)(((
188 [[image:1585305057106-892.png]]
189
190 (Wall)
191 )))|(% style="text-align:center; width:103px" %)(((
192 [[image:1585305040089-504.png]]
193
194 (Wall)
195 )))|(% style="text-align:center; width:106px" %)[[image:1585305076183-264.png]]|(% style="text-align:center; width:103px" %)[[image:1585305036411-105.png]]
196 |(% style="width:258px" %)**//Reactions//**|(% style="text-align:center; width:140px" %)[[image:1585304997147-692.png]]|(% style="text-align:center; width:119px" %)[[image:1585305006797-464.png]]|(% style="text-align:center; width:103px" %)[[image:1585305051638-172.png]]|(% style="text-align:center; width:106px" %)[[image:1585305041630-253.png]]|(% style="text-align:center; width:103px" %)[[image:1585305080279-798.png]]
197 |(% style="width:258px" %)**//Connection forces//**|(% style="text-align:center; width:140px" %)[[image:1585304999104-698.png]]|(% style="text-align:center; width:119px" %)[[image:1585305005051-656.png]]|(% style="text-align:center; width:103px" %)[[image:1585305048862-251.png]]|(% style="text-align:center; width:106px" %)[[image:1585305043262-421.png]]|(% style="text-align:center; width:103px" %)[[image:1585305122539-422.png]]
198 |(% style="width:258px" %)**//Bar internal forces//**|(% style="text-align:center; width:140px" %)(((
199 [[image:1585305000780-455.png]]
200
201 (Beam)
202 )))|(% style="text-align:center; width:119px" %) |(% style="text-align:center; width:103px" %) |(% style="text-align:center; width:106px" %)[[image:1585305053297-144.png]]|(% style="text-align:center; width:103px" %)[[image:1585305119823-907.png]]
203 |(% style="width:258px" %)**//Shell internal forces//**|(% style="text-align:center; width:140px" %)(((
204 [[image:1585305002389-571.png]]
205
206 (Plate)
207 )))|(% style="text-align:center; width:119px" %)(((
208 [[image:1585305045794-448.png]]
209
210 (Wall)
211 )))|(% style="text-align:center; width:103px" %)(((
212 [[image:1585305047435-734.png]]
213
214 (Wall)
215 )))|(% style="text-align:center; width:106px" %)[[image:1585305116143-730.png]]|(% style="text-align:center; width:103px" %)[[image:1585305117975-737.png]]
216 |(% style="width:258px" %)**//Bar stresses//**|(% style="text-align:center; width:140px" %)(((
217 [[image:1585305044592-979.png]]
218
219 (Beam)
220 )))|(% style="text-align:center; width:119px" %) |(% style="text-align:center; width:103px" %) |(% style="text-align:center; width:106px" %)[[image:1585305111733-251.png]]|(% style="text-align:center; width:103px" %)[[image:1585305108274-532.png]]
221 |(% style="width:258px" %)**//Shell stresses//**|(% style="text-align:center; width:140px" %)(((
222 [[image:1585305090155-201.png]]
223
224 (Plate)
225 )))|(% style="text-align:center; width:119px" %)(((
226 [[image:1585305096784-416.png]]
227
228 (Wall)
229 )))|(% style="text-align:center; width:103px" %)(((
230 [[image:1585305100225-317.png]]
231
232 (Wall)
233 )))|(% style="text-align:center; width:106px" %)[[image:1585305103689-525.png]]|(% style="text-align:center; width:103px" %)[[image:1585305106070-791.png]]
234
235 Table: Basic analysis results by FEM-Design Modules
236
237 == Displacements ==
238
239 Depending on the current FEM-Design module, the program calculates and displays the model displacement from linear or non-linear (for RC elements: (% class="wikiinternallink" %)**cracked-section analysis**(%%)) analysis. There are two types of displacement results: translational or rotational. For bar elements, the motion and rotation components can be displayed separately ((% class="wikiinternallink" %)**Detailed result**(%%)) by direction ((% class="wikiinternallink" %)**local axis**(%%)).
240
241 |(% style="width:117px" %)[[image:warning.png]]|(% style="width:1373px" %)(((
242 In [[image:1585305276609-780.png]] //Plate//, the displacements are calculated for the plate regions and beam elements, and the motion is parallel with the global Z direction, so perpendicular to the plate regions. Only reactions can be asked for columns (point reaction) and walls (line reaction).
243
244 In [[image:1585305282360-591.png]] //Wall// and [[image:1585305288140-326.png]] //Plane Strain//, the motion is parallel with the calculation plane of the wall regions.
245 )))
246
247 |(% style="width:105px" %)[[image:light.png]]|(% style="width:1385px" %)Displacement results are recommended to be asked for (% class="wikiinternallink" %)**serviceability load combinations**.
248
249 == Reactions ==
250
251 Depending on the support types, the program calculates the reaction forces and/or moments in the (% class="wikiinternallink" %)**supports**(%%) by direction component, their resultants and the resultant at the support’s center of gravity of line and surface supports.
252
253 |(% style="width:117px" %)[[image:warning.png]]|(% style="width:1373px" %)(((
254 The [[image:1585305276609-780.png]] //Plate// module calculates reactions in columns and walls too above the point/line and surface supports.
255 )))
256
257 The available result components:
258
259 (% class="table-hover" %)
260 |//Fx’ /// //Fy’ /// //Fz’//    |Reaction force in the local x’/y’/z’ axis of the support ((% class="wikiinternallink" %)**group**(%%));
261 |//Fr//|Resultant of the reaction force components (//support group//);
262 |//F//|Reaction force of the (% class="wikiinternallink" %)**single support**(%%);
263 |//Mx’ /// //My’ / Mz’//|Reaction moment around the local x’/y’/z’ axis of the support (//group//);
264 |//Mr//|Resultant of the reaction moment components (//support group//);
265 |//M//|Reaction moment of the //single support//.
266
267 == Connection Forces ==
268
269 Similarly to reactions, the program calculates the forces and/or moments in the connection objects ((% class="wikiinternallink" %)**Edge connection**(%%), (% class="wikiinternallink" %)**Point-point connection**(%%) and/or (% class="wikiinternallink" %)**Line-line connection**(%%)) by direction component and their resultants.
270
271 The available result components:
272
273 // Fx’ / Fy’ /// //Fz’//             - connection force in the local x’/y’/z’ axis of the connection;
274
275 // F           // - resultant of the connection force components;
276
277 // Mx’ / My’ / Mz’//          - connection moment around the local x’/y’/z’ axis of the connection;
278
279 // M//                              - resultant of the connection moment components.
280
281 |(% style="width:90px" %)[[image:1585546946672-302.png]]|(% style="width:1400px" %)The figure shows an example for displaying connection forces at the three connection types. The //Fy'// is displayed at the line (line-line and edge) connections, and the //Fx'// and //Fz'// for the point-point connection. (The color of a result component (e.g. //Fy'//) is the same with the color of the local axis (e.g. //y'//) associated to the component direction) . On the next figure shows the resultants.
282
283 [[image:1585546978369-416.png]]
284
285
286 Figure: Connection forces by connection type
287
288 [[image:1585546985650-610.png]]
289 Figure: The resultants (force and moment) for edge connection and line-line connection forces
290
291 == Local stability results ==
292
293 After calculating the load combinations the Local stability results (Overturning of walls and Sliding) are available in Display results dialog.
294
295 (% style="text-align:center" %)
296 [[image:1585547022222-946.png]]
297
298 (% style="text-align: center;" %)
299 Figure: Display local stability results
300
301 === //Overturning of walls// ===
302
303 Only those walls can be calculated which have at least one horizontal edge in the bottom and edge connection is defined for it. The result is expressed as a percentage:
304
305 * 0% belongs to the case when the vertical force acts at the centre of bottom edges,
306 * 100% belongs to the case when the vertical force acts at one of the corners,
307 * 1000% belongs to the case when the resultant is outside the wall edge.
308
309 [[image:1585547048276-661.png]]
310
311 Figure: Overturning of walls
312
313 |(% style="width:131px" %)[[image:warning.png]]|(% style="width:1359px" %)Overturning of walls results are informative. Without accurate modelling it may lead to incorrect results!
314
315 === //Sliding of edge connections// ===
316
317 The result is the ratio of the design force and the friction capacity. The friction factor can be set in the edge connection dialog.
318
319 [[image:1585547126598-353.png]]
320
321 Figure: Sliding of a wall
322
323 [[image:1585547131510-171.png]]
324
325 Numerical example below will illustrate the //Local Stability//.
326
327 Geometry and Loads
328
329 [[image:1585547154077-678.png]]
330
331 Properties of edge connections
332
333 [[image:1585547161344-140.png]]
334
335 Non-linear calculation (which allows uplift) is recommended to get correct result for local stability.
336
337 [[image:1585547172181-338.png]]
338
339 Displacement graph (as well as connection force) is the easiest way to check the uplift.
340
341 [[image:1585547178112-890.png]]
342
343 === Overturning of wall ===
344
345 With the help of resultants of edge connections, wall’s overturning can be examined as below.
346
347 [[image:1585547188350-275.png]]
348
349 [[image:1585547215701-810.png]]
350
351 [[image:1585547223264-860.png]]
352
353 === Sliding of edge connections ===
354
355 Edge connection’s sliding is calculated in each edge connection //separately// by comparing the x’ component of the connection force as design force, and the limit  force calculated by the y’ components of the connection forces and the friction coefficient of the edge connection.
356
357 [[image:1585547244066-211.png]] [[image:1585547248608-736.png]]
358
359 [[image:1585547266844-316.png]]
360
361 == Bar Internal Forces ==
362
363 The program calculates internal forces and/or moments in the bar elements depending on the applied FEM-Design module.
364
365 The available result components:
366
367 // N//  - normal (axial) force (local x’ axis of the bar element);
368
369 // Ty’ / Tz’//                 - shear force in the local y’/z’ axis direction of the bar element);
370
371 // Mt//                          - torsion moment (around the local x’ axis of the bar element);
372
373 // My’ / Mz’//               - bending moment around the local y’/z’ axis of the bar element.
374
375 |(% style="width:120px" %)[[image:warning.png]]|(% style="width:1370px" %)[[(% class="wikiinternallink" %)**Truss members**>>doc:Manuals.User Manual.Structure definition.Truss member (Geometry).WebHome]](%%) bear only normal forces (N).
376
377 **~ **
378
379 The [[image:1585547397182-463.png]] //Plate// module calculates internal forces only for [[beams>>doc:Manuals.User Manual.Structure definition.Beam (Geometry).WebHome]]. [[Columns>>doc:Manuals.User Manual.Structure definition.Column (Geometry).WebHome]] are point supports.
380
381
382 == Shell Internal Forces ==
383
384 Depending on the current FEM-Design module, the program calculates internal forces and/or moments in the planar structural elements
385
386 The [[image:1585547429886-498.png]] //Plate// module calculates internal forces in the [[(% class="wikiinternallink" %)**plate**>>doc:Manuals.User Manual.Structure definition.Plate (Geometry).WebHome]](%%) regions and in the (% class="wikiinternallink" %)**Global coordinate system**(%%):
387
388 (% class="table-hover" %)
389 | |//Mx’//|bending moment around the **global** **Y axis**;
390 | |//My’//|bending moment around the **global** **X axis**;
391 | |//Mx’y’//|torsion moment;
392 | |//Tx’//|shear force for the global X normal and in the Z direction;
393 | |//Ty’//|shear force for the global Y normal and in the Z direction;
394 | |//M1, M2//|principal moments;
395 | |//M1/M2//|principal moment directions.
396
397 |[[image:light.png]]|Although //Analysis// calculations give results for the **global Descartes system**, internal forces can be asked and displayed in arbitrary (reinforcement) directions by checking (% class="wikiinternallink" %)**design forces**(%%) in case of (% class="wikiinternallink" %)**RC design**.
398
399 The [[image:1585547536999-311.png]] //Wall// module calculates internal forces in the [[(% class="wikiinternallink" %)**wall**>>doc:Manuals.User Manual.Structure definition.Wall (Geometry).WebHome]](%%) regions and in the (% class="wikiinternallink" %)**Global coordinate system**(%%):
400
401 (% class="table-hover" %)
402 | |//Nx’//|normal force in the global X direction;
403 | |//Ny’//|normal force in the global Y direction;
404 | |//Nx’y’//|shear force in the global X-Y plane;
405 | |//N1, N2//|principal normal forces;
406 | |//M1/M2//|principal normal directions.
407
408 The [[image:1585547568303-618.png]] //Plane Strain// module calculates only the (% class="wikiinternallink" %)**shear stresses**(%%) in the (% class="wikiinternallink" %)**wall**(%%) regions and in the (% class="wikiinternallink" %)**Global coordinate system**(%%).
409
410 The [[image:1585547574297-800.png]] //3D Structure// module calculates internal forces and moments in the planar object regions (plate and wall) in their local coordinate system:
411
412 (% class="table-hover" %)
413 | |//Mx’//|bending moment around the **local y’ axis** of the region element
414 | |//My’//|bending moment around the **local x’ axis** of the region element
415 | |//Mx’y’//|torsion moment
416 | |//Nx’//|normal force in the local x’ axis of the region element
417 | |//Ny’//|normal force in the local y’ axis of the region element
418 | |//Nx’y’//|membrane shear force
419 | |//Vx’//|shear force for the local x’ normal and in z’ direction
420 | |//Vy’//|shear force for the local y’ normal and in z’ direction
421 | |//M1, M2//|principal moments
422 | |//M1/M2//|principal normal directions
423 | |//N1, N2//|principal normal force
424 | |//N1/N2//|principal normal directions
425
426 == Bar Stresses ==
427
428 FEM-Design calculates the normal stress in bar elements (beams, columns and/or truss members) with the following meaning:
429
430 //Sigma x‘(max)//        - maximal normal stress (tension);
431
432 //Sigma x’(min)//        - minimal normal stress (compression).
433
434 |(% style="width:119px" %)[[image:warning.png]]|(% style="width:1371px" %)The [[image:1585560780742-260.png]] //Plate// module calculates stresses only in beams. Columns are point supports.
435
436 == Shell Stresses ==
437
438 The program calculates stresses in the top, bottom and middle (so called “membrane”) planes of the planar elements. The meaning of top and bottom side depends on the position ([[image:1585560836929-262.png]] //Plate// module) or the (% class="wikiinternallink" %)**local coordinate system**(%%) (3D modules) of a region element.
439
440 [[image:1585560829628-689.png]]
441
442 Figure: The meaning of planes depending on region position
443
444 So, depending on the current FEM-Design module, we get results from the following:
445
446 (% class="table-hover" %)
447 | |//Sigma x’, top//|normal stress from //Nx’// in top plane
448 | |//Sigma x’, membrane//|normal stress from //Nx’// in membrane plane
449 | |//Sigma x’, bottom//|normal stress from //Nx’// in bottom plane
450 | |//Sigma y’, top//|normal stress from //Ny’// in top plane
451 | |//Sigma y’, membrane//|normal stress from //Ny’// in membrane plane
452 | |//Sigma y’, bottom//|normal stress from //Ny’// in bottom plane
453 | |//Tau x’y’, top//|shear stress from //Nx’y’// in top plane
454 | |//Tau x’y’, membrane//|shear stress from //Nx’y’// in membrane plane
455 | |//Tau x’y’, bottom//|shear stress from //Nx’y’// in bottom plane
456 | |//Tau x’z’//|shear stress (x’ normal and z’ direction)
457 | |//Tau y’z’//|shear stress (y’ normal and z’ direction)
458 | |//Sigma vm, top//|von Mises stress in top plane
459 | |//Sigma vm, membrane//|von Mises stress in membrane plane
460 | |//Sigma vm, bottom//|von Mises stress in bottom plane
461 | |//Sigma 1/Sigma 2, top//|principal stresses and directions in top plane
462 | |//Sigma 1/Sigma 2, membrane//|principal stresses and directions in membrane plane
463 | |//Sigma 1/Sigma 2, bottom//|principal stresses and directions in bottom plane
464
465 |[[image:warning.png]]|(((
466 The x’, y’ and z’ directions are valid in the global coordinate system at [[image:1585561722864-126.png]] //Plate// and in the local coordinate system of planar elements in the 3D modules.
467
468 In [[image:1585561745228-967.png]] //Wall// and [[image:1585561749828-130.png]] //Plane Strain//, stresses are calculated only in the membrane plane.
469 )))
470
471 == Equilibrium Check ==
472
473 The program automatically checks the equilibrium of the analysis calculations. Statical equation is written to the origin [0; 0; 0] of the (% class="wikiinternallink" %)**Global Coordinate System**(%%). It compares the sum of the reactions and the sum of applied loads. Equilibriums can be asked by load case and load combination.
474
475 Just click the [[image:1585561825859-570.png]] //Equilibrium// icon (in Analysis or (% class="wikiinternallink" %)**Design**(%%) mode), choose a load case or load combination to see the equilibrium check results.
476
477 [[image:1585561847367-574.png]]
478
479 Figure: Equilibrium check of Analysis calculations
480
481 If equilibrium error derives from an analysis calculation, the error will be appeared in percentage in the Error column by equation types (force (F) and moment (M)) and directions (x, y and z directions of the global coordinate system). “Error” shows the differences between the resultants of the queried loads and the calculated reactions.
482
483 = {{id name="Analysis for Maximum of Load Combinations and Groups"/}}Analysis for Maximum of Load Combinations and Groups =
484
485 Choosing //Load combinations// for Analysis automatically generates results for the maximum of load combinations too.
486
487 If you define (% class="wikiinternallink" %)**Load groups**(%%) and choose //Maximum of load groups// for Analysis, FEM-Design calculates maximum/minimum results (in all finite element nodes) from the most unfavorable combinations of the load groups according to the applied code.
488
489 So, maximum and simultaneous results of (% class="wikiinternallink" %)**displacements**(%%), (% class="wikiinternallink" %)**reactions**(%%), (% class="wikiinternallink" %)**connection forces**(%%), internal forces ((% class="wikiinternallink" %)**bar**(%%) and/or (% class="wikiinternallink" %)**shell**(%%)) and stresses ((% class="wikiinternallink" %)**bar**(%%) and/or (% class="wikiinternallink" %)**shell**(%%)) can be calculated for maximum of load combinations and groups.
490
491 The symbol “+” and “–“ sign the direction of the maximal value in the valid systems: local or global coordinate systems (depend on the current FEM-Design module). Some examples for the meaning of “+” and “-“:
492
493 Displacement:
494
495 //ez’(+)//                  - maximal uplift in global z’ direction in [[image:1585565432608-409.png]] //Plate//,
496
497 // //- maximum motion in the positive direction of element’s local system in 3D modules;
498
499 //ez’(-)//                   - maximal depression in global z’ direction in [[image:1585565440941-678.png]] //Plate//,
500
501 // //- maximum motion in the negative direction of element’s local system in 3D modules;
502
503
504 Internal forces:
505
506 //Mx’(+)//               - maximal bending moment around the y’ axis (global/local) in positive direction (= same direction with the axis direction).
507
508 //Mx’ (-)//               - maximal bending moment around the y’ axis (global/local) in negative direction (= opposite direction to the axis direction).
509
510 The next figure shows the meaning of simultaneous results.
511
512 [[image:1585565787021-414.png]]
513
514 Maximal Mx’                                                                  Nx’ belongs to maximal Mx’
515
516 Figure: The meaning of simultaneous results belong to a maximal value
517
518 Combination of //Load cases// that gives the maximum analysis results in //Maximum of load groups// can be listed in tables. Just use the [[image:1585565803591-518.png]] //List// command (//Tools// menu) for the //Maximum of load groups// result data.
519
520 [[image:1585565809559-156.png]]
521
522 Figure: Combination of load cases for maximum of load groups results
523
524 = {{id name="Deflection check for RC, steel and timber bars"/}}Deflection check for RC, steel and timber bars =
525
526 A new checking criteria is available for reinforced concrete, steel and timber bars. Deflection utilization is calculated for //load combinations//, //Maximum of load combinations// and //Maximum of load groups// according to the user defined serviceability limit states.
527
528 This new result type is based on the displacement of the bars and the deflection limitation settings which can be defined by the so-called //deflection lengths//.
529
530 [[image:1585565900021-270.png]]
531
532 In the [[image:1585565905964-204.png]] //Deflection// co//nfiguration// dialog, we can specify the types of load combinations/groups for which the deflection check is performed.
533
534 [[image:1585565926731-870.png]]
535
536
537 //Deflection lengths// are used to define those bar segments, where the deflection checking criteria/limitations are coincide. The “Simply supported” deflection lines are denoted with blue arcs below the bar, the ”Cantilever and column” types are orange and the “not relevant” types are black. Relative and/or absolute limit can be set for each //length// individually. If both are requested the dominant one will be calculated and displayed.
538
539 The first option we can set here is the behaviour of the lengths which affects the calculation method of the deflection. If we choose not relevant for a specific length, it will be excluded from the checking process.
540
541 For the better understanding of the next two options, namely the //Simply supported// and //Cantilever// mode let us consider the following example, a cantilever frame structure.
542
543 [[image:1585565936623-364.png]]
544
545 In the midspan we should use the Simply supported option, where we eliminate the rigid body motions in such a way that we connect the endpoints of the length, and measure the deflections of the middle sections from this imaginary line (red skew line on the picture above).
546
547 |[[image:light.png]]|As a consequence of this method, the deflections of the endpoints are zero, the dominant section is usually at the middle of the length.
548
549 On the cantilever, we would like to use the cantilever mode, where the dominant value of deflection on this length will be the difference between the maximum and minimum absolute deflection (in this example the largest distance from the red horizontal line). For columns the same calculation method is used, the only difference is that the deflection is measured in the horizontal plane (from the green lines).
550
551 |(% style="width:120px" %)[[image:warning.png]]|(% style="width:1322px" %)For columns only this (//“Cantilever and column”//) option is available.|
552
553 [[image:1585566012700-385.png]]
554
555
556 As deflection lengths correspond to only specific bar segments, they are independent on the bars in such a way that they can be longer or shorter than the bar itself. But why is this differentiation so important? The answer can be demonstrated with the following two examples. On the left of the picture below, only one beam is drawn, thus if the Relative limit would be calculated directly from the length of this beam, the results would be misleading.
557
558 In other words, in the //L/?// formula, instead of the length of the midspan or the cantilever, the whole length of the beam would be substituted. Therefore, we need two Deflection lengths to differentiate the //L// in the Relative limit formulae on the midspan and on the cantilever. In addition, the limit value also can differ for the two types of structure according to the National Annexes.
559
560 In the second case (to the right on picture below) imagine that our aim is to design a beam splice and check deflections. Two beams need to be drawn for the steel design, but of course during the deflection check we want to use the summed length of the two beams for the calculation of the relative limit value. For this purpose, we define one Deflection length over the two bars - this way we make correct calculations in both cases without any additional modification on the structure.
561
562 [[image:1585566045189-967.png]]
563
564 It is worth to note that in the second case we had two beams, but in contrary to the buckling lengths, definition and editing of deflection lengths can be performed on such set of beams, which are both parallel and continuous.
565
566 By default, deflection lengths are generated automatically. This procedure first search all the previously mentioned parallel and continuous beams sets, then intersect them with the edges/axes of the structural elements (beams, columns, trusses, plates, walls, line and surface supports) and point supports. In the majority of the cases deflection lengths obtained by this way are reasonable from engineering point of view, but in some cases we may want to modify them. A good example can be a structure consisting of two beams with a horizontal support, which should not be considered in the deflection checking process. The following flow diagram illustrates the modification of the two beams step by step. By default, as we can see in the upper picture, the automatically generated deflection lengths coincide with the beams because they are intersected with the horizontal point support. If we would like to have one deflection length over the two beams, we can draw it between the support groups using the Define tool, similarly to the buckling lengths. By this way, the new length substitutes the original ones!
567
568 [[image:1585566057730-325.png]]
569
570
571 |(% style="width:107px" %)[[image:warning.png]]|(% style="width:1308px" %)Deflection length has its own layer.|
572
573 [[image:1585566078715-848.png]]
574
575 //Deflection check// button becomes active if Load combinations and/or Load groups are already calculated. The utilization results can be displayed from the //New result// dialog.
576
577 |[[image:warning.png]]|The Deflection checking process considers only the straight beams and columns. For beams the deflection is measured along their own local z’ axis, for columns it is measured in the global horizontal x-y plane.
578
579 Results requested for a //Load combination// can be displayed both on the deformed and undeformed shape.
580
581 [[image:1585566093043-275.png]]
582
583 Due to the fact that the limit values of the calculation are controlled by the Deflection lengths, the result is constant along them. In other words we have one (dominant) utilization value for each Deflection length. Results for //Maximum of load combinations //and //Maximum of load groups //are only displayed on the undeformed shape of the structure.
584
585 [[image:1585566101399-508.png]]
586
587 = {{id name="Imperfections"/}}Imperfections =
588
589 Imperfection calculation is run only for steel bar elements of the structure. Users can add imperfections to a structure in two ways:
590
591 * **Imperfection modeled by defining loads (manual)**
592 Place for example horizontal point and line loads on a multi-storey building to model imperfection manually.
593 * **Imperfection calculation according to the formula EC3: 1-1 (automatic)**
594 For load combinations, the program can calculates the probable imperfect shapes in real dimensions from the mode shapes (get from (% class="wikiinternallink" %)**stability analysis**(%%)) according to Eurocode. (% class="wikiinternallink" %)**Second order analysis**(%%) must be run by using imperfection. To do automatic imperfection calculations, activate //Imperfections// and set the required number of the imperfect shapes (//Rqd.// cell) for the load combination which you would like to run imperfection for.
595 [[image:1585566123852-913.png]]
596 Figure: Imperfection calculation by load combination
597 \\For the automatic imperfection calculation you got the buckling shape of the structure with real size in real dimension. Critical parameter assigned to a buckling shape is also available with the following meaning:
598 \\ //critical parameter = critical buckling force/actual load//
599 \\or in other words:
600 if the critical parameter is bigger than 1, the structure or a part of it is sufficient to perform the stability analysis; if it is smaller it is not.
601 If the critical parameters differ a lot between the buckling lengths, the first buckling shape is the critical. If the critical parameter values are close to each other, it is your decision what structural part you check by its shape.
602 \\The factor defines the real imperfect shape, so:
603 \\\\ //imperfect shape in real dimension = factor * buckling shape//
604 \\[[image:1585566211268-838.png]]
605 Figure: Automatic imperfect shape calculation
606
607 |[[image:light.png]]|Before imperfection calculation, it is recommended to set minimum 4-5 **//division numbers//** (finite elements) for bars.
608
609 = {{id name="Stability Analysis"/}}Stability Analysis =
610
611 In 3D modules, global stability of the structure can be analyzed automatically if it is requested. Similarly to (% class="wikiinternallink" %)**Imperfections**(%%), the program calculates buckling shapes together with their critical parameters for selected load combinations.
612
613 To do stability analysis, activate //Stability analysis// and set the required number of the buckling shapes (//Rqd.// cell) for the load combination which you would ask stability results for.
614
615 If the //Rqd. as positive// is checked, program will calculate as many stability shapes as necessary to get required number of shapes with positive critical factor. Since it is an iterative method, maximum number of iteration steps can be set by the User in Max no. of iteration cell.
616
617 [[image:1585566484604-695.png]]
618
619 Figure: Stability analysis by load combination
620
621 As result, you got the buckling shape(s) of the structure with unit dimension. The greatest displacement value of the buckling shape is 1 and the others are the ratio of that.
622
623 Critical parameter assigned to a buckling shape is also available with the following meaning:
624
625 (% style="text-align: center;" %)
626 //critical parameter = critical buckling force/actual load//
627
628 or in other words:
629
630 if the critical parameter is bigger than 1, the structure or a part of it is sufficient to perform the stability analysis; if it is smaller it is not.
631
632 [[image:1585566527455-423.png]]
633
634 Figure: Buckling shape calculation
635
636 The last three columns shows the probability of the buckling shapes are global or local, where //eH //meant for horizontal displacement, //eV// for vertical displacement (global Z direction) and //rZ// for rotaion around global Z axis.
637
638 |(% style="width:66px" %)[[image:1585566587364-622.png]]|(% style="width:1424px" %)(((
639 In the example below, the //eH// value of the first shape is 89%, which means it is probably a global buckling shape with horizontal displacement.
640 )))
641
642 (% style="text-align:center" %)
643 [[image:1585566779077-490.png]]
644
645 Displaying the result (see the leftmost inset above) and examining the buckling shape shows that this is indeed a case of global buckling with the horizontal displacement of the frame’s top.
646
647 The same structure’s second shape possesses a very high //rZ// value (99%), meaning this almost certainly is a global torsional buckling shape (shown in the middle inset).
648
649 The fourth shape’s //eH, eV //and// rZ// values are significantly lower, which implies it is a local buckling shape. As the rightmost inset shows, the assumption was correct (local buckling of both columns).
650
651
652 |[[image:warning.png]]|Higher probability values shows high probability that the shape is global. If there are not enough shapes calculated, none might be global.
653
654 |[[image:light.png]]|Before stability analysis, it is recommended to set minimum 4-5 (% class="wikiinternallink" %)**division numbers**(%%) (finite elements) for bars.
655
656 = {{id name="Eigenfrequencies"/}}Eigenfrequencies =
657
658 == Mass/Vibration shape ==
659
660 FEM-Design can do dynamic analysis by calculating vibration shapes of the structural model and the belonging eigenfrequencies and free vibration time values (periodic time).
661
662 To do dynamic calculation, activate Eigenfrequencies and just set the required number of the vibration shapes (Number of shapes cell), the active masses in X, Y or Z direction and the Top of substructure.
663 There is an option to semi-automate calculate the number of shapes to fulfill the 90% horizontal effective mass criteria with the Try to reach 90% of horizontal effective mass. One has to set the starting number of shapes, then the program will calculate them and will check if 90% rule is passed. If it’s not, the program will calculate more shapes and checks the rule again in another iteration. There are two possible ways to end the calculation:
664
665 * The 90% total effective mass is reached in horizontal direction
666 * The maximum iteration number is reached
667
668 (% style="text-align:center" %)
669 [[image:1585566873054-101.png]]
670
671 (% style="text-align: center;" %)
672 Figure: Dynamic calculation
673
674 |(% style="width:119px" %)[[image:warning.png]]|(% style="width:1371px" %)(((
675 Dynamic calculation requires (% class="wikiinternallink" %)**masses**(%%) to be predefined.
676
677 (% class="wikiinternallink wikiinternallink wikiinternallink wikiinternallink wikiinternallink" %)**Seismic analysis**(%%) needs the eigenfrequencies calculations.
678 )))
679
680 In Calculation / Eigenfrequencies dialog the user can set the level of top of the substructure. The masses will be neglected __at__ and __under__ this level.
681
682 [[image:1585566963747-898.png]]
683
684 [[image:1585566974017-250.png]]
685
686
687 In the mass centre of the masses the total mass is displayed with red circle.
688
689 |(% style="width:111px" %)[[image:light.png]]|(% style="width:1379px" %)To get the whole structure’s mass centre position set the level of the Top of the substructure a bit under the structure.
690
691 |[[image:light.png]]|(((
692 This function is useful to neglect the foundation mass in the eigenfrequency calculation so the total mass contribution in Modal analysis can reach >=90%.
693
694 Results of Eigienfrequencies calculation:
695
696 //Masses//                   - mass matrix of (% class="wikiinternallink" %)**point masses**(%%) and/or (% class="wikiinternallink" %)**masses calculated from load cases**(%%) converted into finite element nodes;
697
698 //Vibration shape//  - vibration shape and associated eigeinfrequency (//Frequency//) and periodic time (//Period//).
699 )))
700
701 |(% style="width:109px" %)[[image:light.png]]|(% style="width:1381px" %)(((
702 Before dynamic analysis, it is recommended to set minimum 4-5 (% class="wikiinternallink" %)**division numbers**(%%) (finite elements) for bars.
703 )))
704
705 == Shear center result ==
706
707 FEM-Design can calculate //Shear centers// for each storey of a building. The figures below show a shear center result of an Eigenfrequency calculation.
708
709 |[[image:warning.png]]|(((
710 For displaying shear center, diaphragms are needed for every storey.
711
712 [[image:1585567150564-165.png]][[image:1585567157139-355.png]]
713 )))
714
715 |[[image:warning.png]]|Each displayed shear center represents the result of a calculation based on the storeys below that storey. For example, the calculation of the center displayed on “Storey 2” takes also “Storey 1” and “Foundation” into account.
716
717 [[image:1585567210762-613.png]]
718
719 Shear center results can be listed in //List tables dialog/Analysis/Eigenfrequencies/Shear center.//
720
721 [[image:1585567229877-565.png]]
722
723 [[image:1585567234356-994.png]]
724
725 = {{id name="Seismic Analysis"/}}Seismic Analysis =
726
727 == Methods ==
728
729 In the [[image:1585302865594-127.png]] and [[image:1585302871135-454.png]] modules, seismic calculation offers the following methods to the users according to Eurocode 8.
730
731 * **Modal response spectrum analysis (“Modal analysis”)**
732 * **Lateral force method / Equivalent static load method**
733 This method can be used to calculate the seismic effect in horizontal plan, x’ and/or y’ direction. The main point is to calculate “base shear force” taking into account the base vibration period and design spectrum in x’ or y’ direction, which is distributed into those nodes of the structure where there are nodal masses. The “base shear force” formula is taken from //EC-8 4.3.3.2.2(1)P//. The “base shear force” is nothing else than the total seismic force of inertia that acts between the ground and the structure, and it can be distributed in two ways:
734 ** **Linear shape method (Static, linear shape)**
735 The distribution of the “base shear force” happens according to a simplified fundamental mode shape, which is approximated by horizontal displacements that increased linearly along the height.
736 ** **Mode shape method (Static, mode shape)**
737
738 See the detailed description and the applied theory of all calculation methods in the //Theory book//. This guide introduces only the user interface and the steps of seismic analysis.
739
740 == Steps of Seismic Calculation ==
741
742 The suggested steps of seismic calculation are the followings:
743
744 1. **Mass definition**
745 To calculate the seismic effect, it is necessary to know the vibration shapes and corresponding periods (except the //Static, linear shape// method). To perform dynamic calculations, it is necessary to define mass distribution which can be defined as (% class="wikiinternallink" %)**concentrated mass**(%%) or (% class="wikiinternallink" %)**load case-mass conversion**(%%).
746 1. **Design spectrum definition**
747 The program contains predefined (% class="wikiinternallink" %)**design spectra**(%%) according to //EC8//, but you can also define your own spectra. Use the command (% class="wikiinternallink" %)**Seismic load**(%%) (//Loads// menu).
748 1. **Dynamic calculation**
749 (% class="wikiinternallink" %)**Dynamic calculation**(%%) should be done before performing seismic calculation, which gives sufficient vibration shapes of the structure. Although setup for the seismic calculation can be done at any time, but the seismic calculation could be performed only after //Eigenfrequency// calculation. Run dynamic calculation under //Analysis// by setting the required number of vibration shapes.(((
750 |(% style="width:95px" %)[[image:light.png]]|(% style="width:1355px" %)It is suggested to set the finite element number bigger than 1 at bars (//Finite elements/ //(% class="wikiinternallink" %)**Division number**(%%)).
751 )))
752 1. (((
753 **Settings of seismic calculation**
754 A national code always provides which seismic calculation method has to be performed for different structure, where and when it should be performed and what other effects to be considered (e.g. torsional effect, P-∆ effect). //FEM-Design //provides three types of calculation methods (depending on the applied code):
755 [[image:1585303002015-960.png]]
756 Figure: Settings of seismic analysis
757
758 * **Static, linear shape**
759 As a matter of fact, eigenfrequency calculation is not necessary for this method, because giving the base period time in //x’// and //y’// directions (//Tx’// and //Ty’//) is enough for the calculation. Practically, eigenfrequency calculation performs before setting this data, but these data can be defined using experimental formulas as well. Investigation can be done in //x’// or //y’// direction, or both together.
760
761 (% style="width:700px" %)
762 |(% style="width:225px" %)(((
763 [[image:1585303078921-407.png]]
764 )))|(% style="width:472px" %)You may set the calculation direction to be performed by selecting the desired direction. To set the desired //x’-y’// direction, you should give //Alfa// (alfa is the angle between the global //X// and //x’//; see (% class="wikiinternallink" %)**Direction of the horizontal effect**(%%)).  =0.0 means //x’-y’// directions coincide with global //X-Y// directions.
765
766 |(% style="width:107px" %)[[image:warning.png]]|(% style="width:1383px" %)This method is unusable, if the whole foundation is not in same plane or the horizontal foundation is elastic. In these cases, //Static, mode shape// or //Modal analysis// should be used.
767
768 * **Static, mode shape**
769 In this method the distribution of “base shear force” happens according to fundamental mode shapes (base vibration shapes).
770
771 (% style="width:826px" %)
772 |(% style="width:258px" %)(((
773 [[image:1585303183304-641.png]]
774 )))|(% style="width:565px" %)The table shows how to select the base vibration shapes. It contains all mode shapes (//No//), the vibration time (//T(s)//) and effective masses of the mode shapes in //x’// and //y’// directions (//mx’~(%)// and //my’~(%)//). The effective masses are given in a relative form to the total or reduced mass of the structure. The reduced mass means the total mass above the foundation or above the rigid basement. The value of the effective mass refers to how the mode shape responds to a ground motion direction, so the effective mass shows the participation weight of the mode shape.
775
776 //Select// (or double-click on it) one mode shape in //x'// or/and //y'// direction(s) (//mx’ /my’//). (Yellow field color shows the activation.)
777
778
779 |(% style="width:95px" %)[[image:light.png]]|(% style="width:1355px" %)It is recommended to select that mode shape which gives the largest effective mass as the fundamental mode shape.
780
781 |(% style="width:107px" %)[[image:warning.png]]|(% style="width:1383px" %)The calculation of “base shear force” is performed according to the total mass of the structure and not to the effective mass.
782
783 * **Modal analysis**
784 [[image:1585303301268-646.png]]
785 \\The essence of the methodis the calculation of the structural response for different ground motions by the sufficient summation of more vibration shapes. Method gives possibility to take into account full //x'//, //y'// and //z// (=global //Z//) direction investigation.
786 \\In the table, more vibration mode shape could be selected in //x’//, //y’// and //z //directions if necessary. The last row (orange cells) of the table shows that how large is the sum of the considered effective masses compared to the total or reduced mass of the structure in a given ground motion direction.
787
788 (% style="width:823px" %)
789 |(% style="width:95px" %)[[image:light.png]]|(% style="width:725px" %)According to //EC8//, sum of the effective mass of the choosen mode shapes (at least in horizontal direction) should reach 90% of total mass. Additionally every mode shape has to be taken into account where effective mass is larger than 5%.
790
791 |(% style="width:95px" %)[[image:light.png]]|(% style="width:1355px" %)(((
792 If the sum of the effective mass is much smaller than 90%, eigenfrequency calculation should be done for more shapes in order to reach 90%.
793
794 Lots of mode shapes should be ensured to reach the 90% of total mass in vertical direction. It is highly recommended to check the national code, whether it is necessary to examine the vertical effect or it is not.
795
796 The mode shapes which have small effective mass may be neglected, because their effect in result is very small, but calculation time increases.
797 )))
798
799 * **Summation rule by directions**
800 According to the //EC8//, the summation rule in the individual directions can be selected. In all other codes always the //SRSS// rule is used for summation (there is no choice). Read more about //SRSS// and //CQC// summation rules in //Theory book//. If the //Automatic// is selected, the rule selection procedure is as follow:
801
802 (% style="width:843px" %)
803 |(((
804 [[image:1585303517214-464.png]]
805 )))|(% style="width:556px" %)(((
806 -     Always three directions are investigated (if more than one mode shape is selected in a column), where all mode shape is independent from each other or not.
807
808
809 -     If at least one dependent situation exists in a direction, the program automatically uses the //CQC// rule for all mode shape in that direction, otherwise //SRSS// rule is used.
810 )))
811
812 * **Direction of the horizontal effect**
813 Codes generally speak about seismic calculation in //X-Y// directions. These directions give the maximum effect, if the mass and elastic properties of the structure ensure that the calculated mode shapes lay in //X-Z// or //Y-Z// plane. But it is not always achieved in practice.
814 \\To achieve the unfavorable direction, where the results of ground motion are maximum, the program gives the possibility to set //x'//-//y'// direction for the seismic horizontal effect (//Alpha//). The program suggests the //Alfa// value, if you click on //Auto// button. It finds the most unfavorable direction, where any of the //mx’// and //my’// is zero and the other is maximum in the same row (same shape). But, there is a rule: the direction can be ensured only for one mode shape, so the program selects the row where the effective mass is the maximum. If manually definition is chosen, give an angle for //Alfa// and press the button //Set//.
815
816
817 |[[image:1585303554467-548.png]]|(((
818 On the left hand side figure you can see a badly adjusted //x’-y’// direction (//Alpha = 0//). Appling //Auto// button, the program arranges the direction for the 58.5% effective mass //my’// and correct it to 78%.
819
820 [[image:1585303575071-493.png]]
821
822 Figure: Settings of Alpha
823 )))
824
825 * **Effective mass**
826 The modal effective masses can be compared to the total mass or reduced mass at //Eff. mass//:
827
828
829 |(% style="width:128px" %)(((
830 [[image:1585303685867-313.png]]
831 )))|(% style="width:1362px" %)In //FEM-Design// “//Reduced mass//” means the difference between the total mass of the structure and the basement mass. The basement mass is the sum of all masses which lay on the foundation level (set at //Seismic load/ Others//).
832
833 |(% style="width:107px" %)[[image:warning.png]]|(% style="width:1383px" %)(((
834 //EC8// defines the total mass without basement (//Reduced mass//). The effective masses are generally compared to the //Reduced mass//, but this is not valid for the massive basement with elastic foundation. If the above mentioned situation is the case, it might happen that the sum of the effective masses of a column is larger than the 100%.
835
836 It is uninterested in the calculation point of view, that effective masses are compared to the total or the reduced mass, because these values are given in percentage and only gives information, that which mode shape is the fundamental or which shapes are dominant in a given direction.
837 )))
838
839 At //Options//, more calculation properties can be set:
840
841 * **Combination rule**
842 The combination rule of effects in the //x'//, //y'// and maybe //z// directions can be set here. You can choose from two possibilities.
843 * **Consider torsional effect / Consider second order effect**
844 Additional effects can be taken into consideration during seismic calculation. See the detailed description of these effects in //Theory book//.
845
846
847 |(% style="width:107px" %)[[image:warning.png]]|(% style="width:1383px" %)The calculation of both effects needs the definition of (% class="wikiinternallink" %)**storeys**(%%).
848 )))
849 1. **Seismic calculation**
850 After choosing a calculation method and setting its properties, activate first //Seismic analysis// under //Analysis// and then press //OK//.
851
852 == The Results ==
853
854 Besides (% class="wikiinternallink" %)**displacements**(%%), (% class="wikiinternallink" %)**reactions**(%%), (% class="wikiinternallink" %)**connection forces**(%%) and (% class="wikiinternallink" %)**internal forces**(%%), the program calculates the //Equivalent loads// and the “//Base shear force//”. Results can be displayed by vibration shape (selected at calculation settings), from torsional effect, from sums by direction and from the total sum (//Seismic max//). If equivalent loads are displayed, also the “base shear force” appears on screen (in grey color). Torsional moment effect on the whole structure can also be displayed, if torsional effect was taken into consideration during calculation.
855
856 (% style="text-align:center" %)
857 [[image:1585302782102-375.png]]
858
859 (% style="text-align: center;" %)
860 Figure: Results of Seismic analysis
861
862 |(% style="width:107px" %)[[image:warning.png]]|(% style="width:1383px" %)Because of the square combination rule, the results summed by direction (//Sum, x’//, //Sum, y’//, //Sum, z//) and the total sum (//Seismic max//) give only positive values, so absolute maximums. Also, because of combination rule, the displacement components and the internal forces in one point are not simultaneous results.
863
864 == Summary of Static and Seismic Effects ==
865
866 Seismic effect can be combined with static loads in two ways:
867
868 * By defining new (% class="wikiinternallink" %)**load cases**(%%) contain equivalent seismic loads to take them into consideration at analysis or design calculations as real static loads,
869 * By adding the maximum seismic effect to load combinations or load groups.
870
871 === **Seismic loads as load cases** ===
872
873 The //x' //and //y'// directional loads (also torsional moments) equivalent to the horizontal ground motion can be converted to load cases. (% class="wikiinternallink" %)**“Seismic,...”-type load cases**(%%) behave as static loads: they can be combined, they can be added to groups, and they can be taken into consideration at stability, imperfection and design calculations. As you see in the list of load case types, the seismic effects can be considered with positive and/or negative sign.
874
875 (% style="text-align:center" %)
876 [[image:1585302696112-225.png]]
877
878 (% style="text-align: center;" %)
879 Figure: Seismic effect added as load case
880
881 === **Maximum seismic effect in load combinations** ===
882
883 The total, the maximum seismic effect (see //Seismic max// at //Equivalent loads//) can be added to load combinations. Start the command //Load combinations// (//Loads// menu). Apply //Insert case(s)// on a predefined or new load combination, choose “//(Seismic max)//”, define a load factor and press //OK//.
884
885 (% style="text-align:center" %)
886 [[image:1585302666976-738.png]]
887
888 (% style="text-align: center;" %)
889 Figure: Maximum seismic effect added to load combination
890
891 **Maximum seismic effect as load group**
892
893 The maximum seismic effect (//Seismic max//) can also be added to groups in all codes. Define a group as “//Seismic//”. The program automatically takes the “//(Seismic max)//” into consideration with +/- values in the generation of the most unfavorable results.
894
895 (% style="text-align:center" %)
896 [[image:1585302651022-975.png]]
897
898 (% style="text-align: center;" %)
899 Figure: Maximum seismic effect defined as load group
900
901 = {{id name="Footfall analysis"/}}Footfall analysis =
902
903 This calculation method allows for checking the structure's response for an excited vibration.
904
905 The calculation can be started in Analysis/Calculations/Footfall analysis. The settings for the calculation can be found under the Setup.... Here one can select one of the three available methods:
906
907 * Self excitation
908 * Full excitation
909 * Rhythmic crowd load (Load case shall be selected with this method)
910
911 [[image:1585302627089-203.png]]
912
913 |(% style="width:90px" %)[[image:warning.png]]|(% style="width:1400px" %)(((
914 It is important to choose the correct method (**Self excitation**, **Full excitation** or **Rhythmic crowd load**), because the analysis will run according to the selected method, even though it’s possible to define both self excitation regions and full excitation points.
915 )))
916
917 **Results**
918
919 After Footfall calculation, one can check the Eigenfrequency results (masses, vibration shapes), the nodal accelerations and the nodal response factors.
920
921 [[image:1585302576743-662.png]]
922
923 In //Detailed result// one can see the response factor – frequency diagram of a point, if a //Response factor// or //Acceleration// result is shown. Every previously placed point is remembered and named. These points can be deleted with Delete option. Their name and font can be set by //Properties //option.
924
925 [[image:1585302552305-456.png]]
926
927 These results can be listed in Analysis/Footfall analysis.
928
929 = {{id name="Investigate"/}}Investigate =
930
931 If a warning message appears during calculation (e.g. Load mismatch or Finite element mesh problem) there is a possibility to check and fix the error by navigating in the model with //Investigate//.
932
933 The following pictures show a badly defined load and how can the user check and fix the error with //Investigate// function.
934
935 [[image:1585302527723-346.png]]
Copyright 2020 StruSoft AB
FEM-Design Wiki